Cancel
Showing results for 
Search instead for 
Did you mean: 

postprocessor helical

Solution Partner Builder Solution Partner Builder
Solution Partner Builder
Hi

I want to edit my postprocessor in helical toolpath

1. How to edit postprocessor output G-code g01 x y z ?

2. How to edit postprocessor output G-code g02 or g03 x y z i j k ?

thak you
12 REPLIES

Re: postprocessor helical

this is the place in the post to edit the output.  I'm not really sure what you're asking.  What is it you're trying to change from the standard output?

 

Capture 2.PNG

Capture.PNG

Jake Hardwick
CNC Programmer
Senior Aerospace AMT
Production NX8.5.3.3 Beta testing NX10.0.1.4

Re: postprocessor helical

Solution Partner Builder Solution Partner Builder
Solution Partner Builder

ok
In my postprocessor in helical toolpath it output g02 x y z i j k and
I want to edit my postprocessor to output helical toolpath is g01 x y z .

thank you

Re: postprocessor helical

Phenom
Phenom

Helical output is generally "activated" by importing a custom command in the post called "pb_cmd_helix". Inside this there is a proc called MOM_helix_move. This is the event that NX will call for helix moves - not the one in PB for circular. Out of the box - the code then calls the circular move block template directly (doesn't call MOM_circular_move event.) I have seen a post template that has a post builder graphic event for MOM_helix_move also. So - if you haven't done so - enable helical by importing the "pb_cmd_helix.tcl." Then the circle template should allow adjustment of helical output. If you want points - the post will not see circles at all - it is done in the operation.

 

Untitled.jpg

NX12.02
Windows 10 Pro

Re: postprocessor helical

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

If you want G1 motion for helical moves, in PB_CMD_init_helix:

 

set mom_kin_helical_arc_output_mode LINEAR

Ken Akerboom Sr CAx Systems Engr, Moog, Inc.
Production: NX10.0.3.5 MP16/TC11.2
I'd rather be e-steamed than e-diseaseled


Re: postprocessor helical

Solution Partner Builder Solution Partner Builder
Solution Partner Builder
Thank you

now I can not find mom_kin_helical_arc_output_ mode LINEAR in PB_CMD_int_helix please tell me How to set ?

Thak you a lot

Re: postprocessor helical

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

Import the custom command.

Get to Program & Tool path -> Custom commands

Click on "import" button

Navigate to %UGII_ROOT_DIR%\POSTBUILD\pblib\custom_command

select pb_cmd_helix.tcl

"OK" out

Now edit PB_CMD_init_helix

Ken Akerboom Sr CAx Systems Engr, Moog, Inc.
Production: NX10.0.3.5 MP16/TC11.2
I'd rather be e-steamed than e-diseaseled


Re: postprocessor helical

Experimenter
Experimenter

Hi All,

 

Good Day !!!

 

In this same topic I have an issue like..

 

I am creating helix as a sketch (NX8.5)

Then with "Generic motion" operation using follow curve option I am generating toolpath.

I got the tool path as I want. But I am getting only point output not helix not even circular.

 

I do have MOM_helix_move even If I create the same with "Hole milling" operation I am getting helix code.

 

With Generic Motion I am not getting the helix_move.

 

I am adding some prep path before helix thats why I forced to go for Generic motion.

 

Kindly help me to get resolved...

 

Re: postprocessor helical

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

You have to determine where the issue is:

- Does NX's "internal toolpath" have helix data?

- Is the post correctly interpreting that data?

 

List the internal toolpath (if editing the op, right button on very bottom row, otherwise right-click on the operation -> toolpath -> list)

If you see a "CIRCLE/...,TIMES,(number here)"

Then the internal toolpath has helical data.

If all you see is "GOTO/...", then it doesn't. 

If it is all "GOTO" statements, then it is an NX issue, there's not much you can do about it (at least not without a huge amount of tcl code to fit a helix to the "goto" points).  Submit an IR to GTAC, to create an ER to get NX to create helical data for the case your are trying to do.

 

So if the internal toolpath DOES have helical data, you have to determine why the post isn't outputting correctly. 

1) Have you imported the custom commands per the above?

2) is the helix axis not in a "principal plane" (may depend on your machine / post kinematics - if it is a table/table, you should be OK, if there is a head rotary axis, there may be issues)

3) other issues.

 

Ken Akerboom Sr CAx Systems Engr, Moog, Inc.
Production: NX10.0.3.5 MP16/TC11.2
I'd rather be e-steamed than e-diseaseled


Re: postprocessor helical

Experimenter
Experimenter

Thanks for your reply !!!

 

As you said in first case, I am getting GOTO in cls data not CIRCLE..

Learn online





Solution Information